How to couple three different inductor?

[Anup_Barai]

Hi I have three different inductor coil connected three different circuit. They have different mutual inductance. I need to detect voltage response on two inductance when other coil has a supply voltage. Check the attachment for an example circuit.

Thank you in advance.

[Kev_R]

Hi Anup_Barai, 

Thank you for posting to our forum. My name is Kevin and I am an application engineer at NIUK. I am unsure if your question is best placed in this forum, it seems to be a purely electronic question. What NI products are you using to detect the voltage response?

Kind Regards

[johnsold]

Anup_Barai,

You can have multiple inductors mutually coupled in SPICE.  I do not have Multsim, so I cannot verify whether it uses the same method.

My test has two inductors coupled to L1 and three to L2.  This runs on my SPICE program:

Test mutual triple inductor

*

Iin 1 0 DC 0 AC 1

L1 1 0 1u
C1 1 0 200p
R1 1 0 1Meg

L2 2 0 2u
C2 2 0 100p
R2 2 0 500k

L3 4 5 500n
C3 4 5 100p
R3 4 5 1Meg

L13 1 3 25n
C13 3 4 100p
C130 4 0 8p

L23 2 6 8p
C23 5 6 100p
C230 5 0 8p

Rg 5 0 1G

K12 L1 L2 0.8
K13 L1 L3 0.12
K132 L13 L2 0.03
K23 L3 L2 0.13

.END

The results look like this:

The values I chose are arbitrary.  The documentation for my SPICE program indicates that some values of coupling may not be physically realizable.  It does some checking and issues warnings.

The relationaship between mutual inductance and coupling is M = k*sqrt(L1*L2).

Lynn

[OStep]

In Multisim you can couple an arbitrary number of inductors using the same coupling element.

If you are using SPICE directly, the syntax is 

K<anyname> L1 L2 L3 ... Ln <CouplingCoefficient>

L1 L2 L3 and Ln are the instance names of the inductors. A valid line might be:

K1 L1 L2 L3 0.99

You are probably modeling your circuit using the schematic capture tool and hoping to use a graphic approach. This functionality is neatly wrapped up in the INDUCTOR_COUPLING component under Basic>>TRANSFORMER.

You simply specify your inductors by their reference designators, as seen on the schematic, and the coupling coefficient. View the help file for this component to get more details.

Hope that helps.

[Anup_Barai]

Hi Kavin,

For this problem I am using Multisim 12. Long ago I did simulated the circuit attached with my question using multisim 8/9. And now I totally forgot how I did that time and also lost that file.

So I know Multisim is capable to do this.

After Simulation I will use a 60MS/s Digitizer (and probably a FPGA module to do FFT) with PXI System (and Labview). But before I fed the detected signal to the digitizer I need to aplify it. To design this highly phase stable amplifier I need the information what is the dectected signal level.

Hope I made clear my application.

Thank you for your help.

Best regards,

Anup

[Anup_Barai]

Hi Max,

For this problem I am using Multisim 12. Long ago I did simulated the circuit attached with my question using multisim 8/9. And now I totally forgot how I did that time and also lost that file.

So I know Multisim is capable to do this.

INDUCTOR_CUPLING component is my last hope.

Thank you for your help.

Best regards,

Anup